Rover 336 retrofit – horizontal drills and tool offsets in LinuxCNC

Hello,I am currently retrofitting a Biesse Rover 336 with LinuxCNC.The machine is controlled with a Mesa 7i77, and I am using EtherCAT modules distributed throughout the machine for the I/O.Originally the machine had a Control Techniques Unidrive VFD, but I was unable to change the required parameters, so I replaced it with a Danfoss VFD, which is now working well.At this point the machine is mostly operational:

• Homing works
• XYZ motion works
• Spindle runs correctly
• The toolchanger sequence is mostly prepared

So I am approaching the final stages of the retrofit.I am using Probe Basic as the interface.Machine configuration

• Toolchanger: 7 tools
• Vertical drills: ~25
• Horizontal drill (X axis): 1
• Horizontal drills (Y axis): 3

My current plan is:

• Tools 1–7 → spindle toolchanger
• Tools 101–130 → drill bank (fixed tools)

Questions about tool offsetsFor the drill bank I need to determine the XYZ offsets relative to the main spindle.I am unsure what the best way to handle this is.Options I am considering:

1. Store the offsets in the tool table (like normal tools)
2. Apply the offsets inside the M6 tool change routine, since these drills are fixed and it may reduce the chance of mistakes.

Do tool table offsets work correctly for horizontal drills, or is there a better recommended approach?Fusion 360 questionI also created a test piece in Fusion 360 to test the horizontal drills.However I get the following error:
 Error: Function 'positionABC' can only be used with multi-axis machine configurations.
Error at line: 2040
Error in operation: 'Drill2'I suspect this may be related to how I defined the horizontal drilling operation.Is there a recommended way to program horizontal drilling for drill banks in Fusion when targeting LinuxCNC?Any advice from people who have implemented drill banks or horizontal drills on router-style machines would be very helpful.Thanks!

In LinuxCNC, the XYZ tool offsets applied via G43 work correctly for the tool.
You can apply them inside M6 by executing G43 inside remap, or separately — it doesn't matter.



The error you are receiving indicates that you have changed the tool orientation (rotated the WCS). The post-processor checks whether your MachineConfig can perform an ABC coordinate system rotation, but you most likely have a standard 3x configuration.

However, to use drilling in planes other than XY (G17) without WCS rotation, you will need to change the post-processor logic in Fusion 360. The standard LinuxCNC-EMC2 post does not allow this. The standard 5x or 3+2 post will not work either as they rotate the coordinate system, which is unnecessary when drilling in a plane other than g17.

There are different ways to implement this:

1) Classic 5x/TCP rotates the coordinate system by controlling the AB axes and TCP activation codes — this is probably too complicated for your machine.

2) Allow tool vector orientation other than Z – this is often used for rotary/angle heads on milling machines.  To do this, you need to modify the postprocessor. See this topic for more information: forums.autodesk.com/t5/hsm-post-processo...n-stock/td-p/8911668

In this case, you do not need to select 'Tool orientation' in Fusion; WCS remains the same as in the setup.


3) The strange but common logic of posts for some furniture machining centers with drilling blocks that you can find looks like this: the g54 offset is defined for the XY machine plane, other offsets are used for side surfaces, and then the CNC recalculates. The control program looks like a cardboard box unfolded onto a plane. I don't think you'll want to use this strange proprietary logic.


I recommend adding mandatory checks:
In the post-processor:
- Check which tool numbers can be used in planes other than the XY plane.
- Check that side tools (T for the ZY plane) are only used for operations on the ZY work plane.
In the CNC:
- check that the XYZ tool offsets for side tools are not equal to 0 (this check can be performed inside M6).